CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)

 Thomas April 1, 2005 03:02

Hello,

just a short question. When I want to be sure that my solution is converged, then the report->fluxes->total heat transfer rate for all surfaces should sum to zero (or near to zero). Is this right?? Or is there another posibillity to be sure about convergence. In my actuall problem the residuals are all below the fluent default criteria (e.g. 0.001 for conti) The continuity is at about 0.00014, but the total heat flux report is far away from zero.

 Z April 1, 2005 04:12

the fluent defualt criteria is not good in fact you must get the convergnce to 1e-05 level. Z

 Thomas April 1, 2005 04:18

But can I use the flux-report ->total heat transfer rate over all surfaces as a criteria for convergence?

 ap April 1, 2005 07:52

I'd suggest the following:

1. Set the convergence criteria for all variables to a really low value, such 10^-10 or less. Let FLUENT iterate until the residuals flatten and stay stable.

2. Check the mass and energy balances using the Report->Fluxes panel.

Best regards, ap

 Jason April 1, 2005 08:00

Not sure if you're doing this, but you can use a volume monitor and monitor the heat flux during iteration. I recommend monitoring the convergence of any values you hope to get out of the solution (like if you're interested in a wall temperature, I'd make a point where you think the maximum temperature is and monitor the temperature at that point). You can monitor just about anything, but you might have to create a surface, line, or point in Fluent to monitor the value.

Hope this helps, Jason

 major April 2, 2005 10:05

Hello,Jason: Besides monitor the residuals. I monitor the velocity of a point in the solution domain. I don't know the velocity value of this point before calculation. When the velocity reach a constant,I think it is the converged solution.

 ap April 2, 2005 15:20

Regards, ap

 Sham April 8, 2005 19:38

I agree with Jason. Are you solving steady of unsteady problem? Anyway here are soem guides for you and I got this from Dr Ben Simpson of Fluent Australia.

Usually on a steady problem convergence is judged either by 3 order drop in the residuals, or the residuals going flat (flat lining), or mass fluxes balance (report-integral-mass_flux, balance should be 3 orders of magnitude lower than inlet flux), or by monitoring flow characteristics for changes (such as drag, lift or velocity at a certain point) or most likely a combination of them all.

If a problem is transient, meaning the flow is changing with time, then these same criteria are used but to judge whether the solution has converged at each time step. Most users running transient simulations just check the residuals and see if either they are dropping 2-3 orders each time step or that they are flat-lining.

Finally if a transient problem 'converges' over time, then by definition it is a steady problem and should be run as one. If you find that your problem is not converging every timestep then try either increasing the number of iterations per timestep or decreasing the timestep size.

Finally ...*.Note* it is quite common that when running transient simulations that the fluent built in '3 order of magnitude' convergence check will never be reached each time step. This automatic convergence check is only a guide. What you have to remember is that by definition a residual is a measure of the difference in solution between one iteration and the next (i.e. a measure of the error in the solution).

If you have fairly small timesteps then the solution is not changing very much between timesteps. Therefore the residuals will not fall very much and the 3 order of magnitude drop will never be met. What I normally do is turn off the automatic check (toggle of the button on each residual) and then run for a set no. of iterations per timestep. If the residuals do not flat line at each time step, then increase the fixed number of iterations per timestep.

Hope this will help.

Sham.

 All times are GMT -4. The time now is 20:13.